This tutorial guides you through the process of using CAM Assist's ‘3+2 Axis’ machining mode, with a ‘User-defined' machining direction, to compute a toolpath strategy for a part.
When using the ‘User-defined’ machining direction:
The tool orientation comes from the orientation you specify in the Target setup(s) within CAM Assist.
A toolpath strategy will only be computed by limiting the tool to the specified orientation.
Facing operations will only be computed if the +Z Axis is selected.
The tool then operates on the part from a fixed orientation, which means that the orientation cannot change during cutting.
This tutorial uses CloudNC’s ‘Demo Part 1’. However, the same process can be used for any part that can be opened in Siemens NX.
CAM Assist works with the Siemens NX manufacturing environment and manufacturing templates.
Preparation
Before following this tutorial, you must have successfully completed the following steps:
Install CAM Assist - follow the instructions in Installing CAM Assist.
Open a part - follow the instructions in Opening a Part (this tutorial uses ‘Demo Part 1’).
Open the ‘CAM Assist’ menu - it contains the CAM Assist ribbon shown in the screenshot to the right.
Click CloudNC CAM Assist - in the CAM Assist ribbon.
Using the ‘3+2 Axis’ Machining mode
On completing the Preparation, you’ll see the CAM Assist user interface with ‘Demo Part 1.prt’ open, as shown below.
To use the ‘3+2 Axis’ Machining mode with a ‘User-defined’ machining direction, you’ll take the following steps:
Specify the Machining mode
For Machining mode, CAM Assist provides you with two options: ‘3 Axis’ and ‘3+2 Axis’.
Check the box for 3+2 Axis
Specify the Machining direction
For machining direction, CAM Assist providers you with three options: ‘Aligned to X, Y, Z axes’, ‘User-defined’, and ‘Automatic’.
Check the box for User-defined
Configuring the Target setups
The content of the ‘Target setups’ section reflects the workpiece configuration of the part, as displayed in the ‘Geometry’ view of the Siemens NX Operation Navigator (as shown below).
Check the Setup(s)
Within CAM Assist, the ‘Target setups’ are numbered sequentially, in the same order as in NX’s Geometry view.
You’ll notice that ‘Demo Part 1’ has two Target setups: ‘Setup 1’ and ‘Setup 2’.
If you want CAM Assist to create a toolpath strategy for a setup, ensure its respective checkbox (Setup 1/Setup 2) is checked.
Check the box for Setup 1
Check the box for Setup 2
Same direction for roughing and finishing
The content of the ‘Target setups’ section changes depending on whether ‘Same direction for roughing and finishing' is checked or unchecked.
The side-by-side screenshots below show these changes.
‘Same direction for roughing and checking’ is checked. Checking the box indicates you want the part to be machined using the same direction for both roughing and finishing operations. |
 |
Note the option for:
This is used to specify the machining direction for roughing and finishing (see below) |
‘Same direction for roughing and checking’ is unchecked. Unchecking the box indicates you want the part to be machined using different directions for the roughing and finishing operations. |
 |
Note the options for:
These are used to specify different directions for roughing and finishing (see below). |
Specifying the same direction for roughing and finishing
At this point in the tutorial:
For Setup 1 - check the box for Same direction for roughing and finishing.
You’ll configure Setup 2 later on in the tutorial.
The ‘Select machining directions’ icon (see the image to the right) is used to indicate the roughing and finishing direction by clicking on a face on the part, within Siemens NX, that is perpendicular to the machining direction.
Click the Select machining directions icon
Within Siemens NX:
Click on the face of the model/part that is perpendicular to the direction that will be used for roughing and finishing.
Two things happen when you click on a face (as shown in the image to the right):
In Siemens NX - the face is highlighted.
In CAM Assist - ‘Select machining directions (0) changes to ‘Select machining directions (1)’.
A green tick is shown to indicate a valid selection has been made.
That’s it, you have specified the same machining direction for roughing and finishing.
Specifying a different direction for roughing and finishing
Next, for this tutorial:
For Setup 2 - uncheck the box for Same direction for roughing and finishing.
With the box unchecked, you'll have to specify the roughing direction and the finishing direction separately.
First, the roughing direction…
The ‘Select roughing directions’ icon (see the image to the right) is used to indicate the roughing direction by clicking on the part's face, within Siemens NX, that is perpendicular to that direction.
Click the Select roughing directions icon
Click on the face of the model/part that is perpendicular to the direction that will be used for roughing.
Two things happen when you click on the face (as shown in the image to the right):
In Siemens NX - the face is highlighted.
In CAM Assist - ‘Select roughing directions (0) changes to ‘Select roughing directions (1)’.
A green tick is shown to indicate a valid face has been selected.
You can click on more than one face.
Within CAM Assist:
Next, the finishing direction…
The ‘Select finishing directions’ icon (see the image to the right) is used to indicate the finishing direction by clicking on the part's face, within Siemens NX, that is perpendicular to that direction.
Click the Select finishing directions icon
Click on the face of the model/part that is perpendicular to the direction that will be used for finishing.
Two things happen when you click on the face (as shown in the image to the right):
In Siemens NX - the face is highlighted.
In CAM Assist - ‘Select finishing directions (0) changes to ‘Select finishing directions (1)’.
A green tick is shown to indicate a valid face has been selected.
You can click on more than one face.
Set the Avoidance Geometry
Specifying Avoidance Geometry is an optional step
For details and step-by-step instructions, see the tutorial ‘Using Avoidance Geometry’.
Keep roughing order
The checkbox could be:
Checked - tool orientations will be ordered in the same sequence as they are selected (this applies to ‘Select roughing directions’, see below).
Unchecked - tool orientation will be sequenced by CAM Assist but may not be in the order selected.
For ‘Setup 1’ and ‘Setup 2’
Check the box for Keep roughing order icon
Set the Workholding security
CAM Assist will choose roughing tools suitable for the specified workholding.
Set the slider to the required position between the two extremes:
Excellent - a more secure ('excellent') workholding, such as a vise with serrated jaws, will result in CAM Assist selecting larger tools or more aggressive cutting parameters. This will result in faster toolpaths, but with more force on the workpiece.
Poor - a less secure ('poor') workholding, such as a thin part held by a soft jaw, will result in CAM Assist selecting smaller tools or less aggressive cutting parameters. This will produce slower toolpaths, but with less force on the workpiece.
For ‘Setup 1’ and ‘Setup 2’
Set the Workholding security slider to 'Excellent’.
Examining CAM Assist’s other tabs
Before clicking OK, it’s a good idea to examine the other tabs to ensure that the requirements for CAM Assist’s tool strategy are fully configured:
Click OK.
On clicking OK, CAM Assist closes and computes a toolpath strategy, which is displayed within the ‘Program Order View' of Siemens NX’s Operation Navigator (as illustrated in the following screenshot).
